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Flat pattern sheet metal drawing

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Flat pattern sheet metal drawing

Hello,

 

When creating a drawing of a sheet metal part, we currently use the family table method to have two models in one sheet. We would prefer not to use this method as it introduces an extra part number that we must track. We have tried using simplified reps however, this means all parent assemblies must have a simplified rep as well!

 

Does anyone have an alternative to using family tables that will allow us to put a flat pattern view into a drawing without using simplified reps? Either that or being able to change the master rep to exclude a feature.

 

Any help would be grateful.

 

Regards,

Hannah

 

P.S We are using Creo Parametric 1.0

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1 ACCEPTED SOLUTION

Accepted Solutions

Re: Flat pattern sheet metal drawing

I worked with it some more.

It really is a lesson in how the Display States works along with Simplified Reps (I didn't realize they were dependent). Always good to learn something new.

In short, I was able to flatten and then bend back the flange. Using proper technique in Excluding features will get you the Display States you need for the drawing -and- have the default be the master you want. It does cause features to fail regeneration but once they too are excluded from the simplified rep, these do not cause overall regen failures. The requirement you are looking for also comes with the price of thoughtful tree management and associativity. Nothing new, of course.

I think I've also run into a few bugs along the way, like the drawing views not following the default drawing scale. But that's another thread.

DisplayState3.PNG

25 REPLIES 25

Re: Flat pattern sheet metal drawing

Here is a movie I created for the purpose. It was created in WF5. Could be similar in Creo 1.0. With this method, the flat state is Automatically created in the family table. Further, it is always the LAST feature. Meaning any feature added after creation of Flat state would be put before the flat state by the software.

Video Link : 3236

Re: Flat pattern sheet metal drawing

Thank you for the response, unfortunately, Creo does not have the same menus. I am also trying to avoid family tables for sheet metal as it would require a separate part. We would like one part number/name for the drawing and the sheet metal component. From this single part we would like to be able to place two different drawing views - flat and assembled. As stated above, we were unsuccessful using simplified reps and are trying to find a better option.

Re: Flat pattern sheet metal drawing

You are looking for Combined States.

It is a bit convoluted but I believe this was added for the very reason you are looking for.

Here is a simple metal part showing it in a bent state and unbent state.

DisplayState1.PNG

DisplayState2.PNG

The idea is that you create a new view state as seen on the model lower graphics edge. Bent/Unbent/Default

While in that state, you can edit the visibility of a feature in the tree

In the drawing, when inserting a general view, it asks which Combined State you wish to use.

This is Creo 2.0. Let me know if you want the files.

Highlighted

Re: Flat pattern sheet metal drawing

Hi Antonius,

Thanks for your response! It seems like this method is similar to creating simplified reps, and will cause a problem when assembling a sheet metal part. As the default view is to have all features included, it would mean that when you add a sheet metal part to an assembly, it will be the flat pattern. As the majority of our sheet metal parts are used in larger assemblies, this method would not resolve the issue we are having.

Is there a way to view the flat pattern without creating a feature? There is the flat pattern previewer however, you cannot do anything with this preview view...

Regards,

Hannah

Re: Flat pattern sheet metal drawing

Oops, of course. What if you forget the unbend and "Exclude" the bend operations? This may mean some issues if features are added after bending.

I also tried "Bend Back" but feature failed. I rarely use the sheetmetal extension so I need to understand its limitations better.

Re: Flat pattern sheet metal drawing

I worked with it some more.

It really is a lesson in how the Display States works along with Simplified Reps (I didn't realize they were dependent). Always good to learn something new.

In short, I was able to flatten and then bend back the flange. Using proper technique in Excluding features will get you the Display States you need for the drawing -and- have the default be the master you want. It does cause features to fail regeneration but once they too are excluded from the simplified rep, these do not cause overall regen failures. The requirement you are looking for also comes with the price of thoughtful tree management and associativity. Nothing new, of course.

I think I've also run into a few bugs along the way, like the drawing views not following the default drawing scale. But that's another thread.

DisplayState3.PNG

Re: Flat pattern sheet metal drawing

Thanks for the answer! I think this solves our issue though I could not get it to bend back once creating the flat pattern - it seems to always remain as the last feature. However, it seems that unbend does the same thing as flat pattern, and then I can bend back. From this I can create a simplified rep of the flat pattern while maintaining the assembled version as the master.

Thank you so much for the thoughtful answers!

Re: Flat pattern sheet metal drawing

I am glad you found a workable solution.

As I stated above, my first unbend failed after the flatten on the original session, and when I went back to it is in a new session, it worked fine. It could have something to do with what Creo "thinks" is pre-selected or just a bug.

If I worked with this a lot, I would probably ferret out the problems and report them. It is yet another very powerful command that is finicky to work with.

Now that M020 is out for Creo 2.0, I might give it another go.

Re: Flat pattern sheet metal drawing

Hello,

please tell me the trick how did you put UNBEND feater after FLAT PATTERN feater? Using Creo 2.0 M070. Like ProE help says: The Flat Pattern feature remains the last feature in the Model Tree and maintains the flat model view. The flat pattern is suppressed when you add or redefine features in a design. It is automatically resumed after the features have been added.

flat_pattern.jpg

l´m trying to solve thise problem in our company. My idea is:

1) Use Flat pattern --- it gives SMT_FLAT_PATTERN_LENGTH & SMT_FLAT_PATTERN_WIDTH parameters.

2) Use thise parameters from flat pattern like overral dimmensions of sheet (width x length x thick)

3) Use simplified represenation method --- exclude band back feater for flat state.

4) Don´t use FT because you need add more models in drawing --- bad manage.

Only problem is: How to put band back after flat pattern feater?